So I had gotten quite far milling this part out of 6061-T6 bar stock. Was at first using a 4 flute carbide with AlTiN coating. Obviously gummed up without lubricant quite easily. Switch to a 3 flute from Lakeshore Carbide with ZrN coating. Chatter was less but still there. Milled fine dry until it got deep enough in the outline slot cut. The aluminum gummed up the bit while it was moving at a good pace and that's the reason for the big gouge in the part. Broke several v wheels in the process. So I'm thinking the end mill is rubbing both sides of the slot more and more with every pass creating friction and heating the metal. Would a contour cut with multiple stepovers be the solution? Or am I not getting enough chip evacuation? Your thoughts?

As gummy as aluminum is my gut says follow Will's advice with the wider slot and I would give a 2 flute end mill a shot. If you need really good surface finish. Leave a bit of Aluminium at the bottom(one or 2 passes) and a couple of thousands on the part and do a cleanup pass with the three flute. That way the three flute isn't rubbing the whole length on one side. I didn't see what software you were using, I know in Fusion there is an option to make the slot 2 passes wide, it takes the outside pass first then moves round to the part side to help with rubbing in deep parts.

CrazyBillybob wrote:As gummy as aluminum is my gut says follow Will's advice with the wider slot and I would give a 2 flute end mill a shot. If you need really good surface finish. Leave a bit of Aluminium at the bottom(one or 2 passes) and a couple of thousands on the part and do a cleanup pass with the three flute. That way the three flute isn't rubbing the whole length on one side. I didn't see what software you were using, I know in Fusion there is an option to make the slot 2 passes wide, it takes the outside pass first then moves round to the part side to help with rubbing in deep parts.

looks like your 85% of the way there..

Good Luck,
CBB

I'm using Fusion 360 for CAM. I'll have to give a two flute a try but I like the rigidity a three flute has.

A couple other options are try turning on helical in the slotting tab in 360 this would put less of the tool in contact at the cutting area. The other option is create an outline 1.5- 2X the width of you tool from the outside of the part 1/2 or 2/3 the thickness of your part do a 2D adaptive on it. Then finish up with your slotting on the last 1/4-1/3. This keeps the tool from rubbing the whole length of tool, in theory this should cut down on the side loading and thus tool deflection at the bottom of the pocket.

Again best of luck. Please let us know what you do to pull this off. (I have a couple projects that I need to make exhaust and /or intake flanges for in the future).

CBB

(not sure if you can apply this but figured there's never to much info. <-- I have no affiliation with this channel just like some of his stuff)

CrazyBillybob wrote:A couple other options are try turning on helical in the slotting tab in 360 this would put less of the tool in contact at the cutting area. The other option is create an outline 1.5- 2X the width of you tool from the outside of the part 1/2 or 2/3 the thickness of your part do a 2D adaptive on it. Then finish up with your slotting on the last 1/4-1/3. This keeps the tool from rubbing the whole length of tool, in theory this should cut down on the side loading and thus tool deflection at the bottom of the pocket.

Again best of luck. Please let us know what you do to pull this off. (I have a couple projects that I need to make exhaust and /or intake flanges for in the future).

CBB

(not sure if you can apply this but figured there's never to much info. <-- I have no affiliation with this channel just like some of his stuff)

I've been watching a lot of his videos before taking on this project, that's how I learned to use fusion 360. I found a way to make the slot with extra stepovers before continuing on the stepdown, but I think an air blast setup might be needed to help in keeping the slot clean.

when it gums up it's the aluminum melting. everything about machining metal is about controlling the heat. the thinner the material the less of a conduit it has to evacuate heat and the larger chance it has to start melting to the bit. also chip evacuation is key, they have already been cut so they contain a lot of heat and have nowhere to distribute the heat to so the next time the cutter digs into them they with melt to the bit and gum it up. at the bare minimum you want air blowing on the bit to carry some heat away and get chips out of the cut while also cooling down any of the chips that dont make it out. lubrication can help by lowering heat from friction. heat is the real enemy

You can use a simple air nozzle to manually blow the chips out. Or you can look at something like this https://www.amazon.com/Coolant-Spray-Sy ... stable+cnc (I have no idea of the quality or performance of this unit ) I know there are some way nicer units out there too. Just guessing that your here means your running with a budget.

Jeremy is right cutting chips a second time, no matter what the material is. Is a good way to dull, blue, break or gum up tooling.
CBB

You could just put tape around the outside of the aluminium piece to build up a bit of a wall, and dump a bit of cutting oil there. It's not all that good for evacuation of swarf, but everything stays cool.
(If you're cutting slowly you may be able to use a plastic knife or a spatula to scrape away swarf here and there.)